Translating an Abaqus Substructure to an MSC.Adams Flexible Body

The abaqus adams translator converts an Abaqus substructure to a flexible body in a format that can be used by the MSC.Adams multibody dynamics code.

The translator reads Abaqus data from a substructure SIM file and writes data to an MSC.Adams modal neutral (.mnf) file.

This page discusses:

See Also
About Execution Procedures
In Other Guides
Translating Abaqus data to modal neutral file format for analysis in MSC.ADAMS

Products Abaqus/Standard

Using the Translator

The following procedure summarizes the typical usage of the abaqus adams translator:

  1. Create an Abaqus substructure. (General guidelines for building Abaqus models with substructures are described in Using Substructures.)

    The substructure generation step must write at least the mass and stiffness matrices. It can also write the recovery and viscous damping matrices. The FLEXIBLE BODY option must be used. For example, 

    SUBSTRUCTURE GENERATE, MASS MATRIX=YES, RECOVERY MATRIX=YES, VISCOUS DAMPING MATRIX=YES
FLEXIBLE BODY, TYPE=ADAMS

    • If TYPE=ADAMS, a flexible body including all high-order inertia invariants is created.

    • If TYPE=ADAMS, FORMULATION=REDUCED, a simplified flexible body (without high-order inertia invariants I5 and I9) is created.

    In addition, you can add the following data to translate stress and/or strain: 
    ELEMENT RECOVERY MATRIX, POSITION=AVERAGED AT NODES
S,
E,

    If the Abaqus analysis did not use SI units (meters, kilograms, Newtons, and seconds), you must define units when you run the translator using the length, mass, force, and time command line options. If the Abaqus analysis uses American or English units (inches, pounds force, and seconds), the mass unit is slinch.

  2. Run the Abaqus analysis.

  3. Run the abaqus adams translator to read the substructure SIM database produced by the analysis and to create the modal neutral file.

Translating Modes with Negative Eigenvalues

Typically, for a nonprestressed, unrestrained substructure in three dimensions, you expect to find six rigid body modes with associated zero eigenvalues. The situation is, in general, different for prestressed substructures, which may have fewer than six modes with zero eigenvalues. Prestressing may change some expected zeroes into values that are significantly positive or negative, depending on the sign of the prestress.

By default, the translator deletes modes with negative eigenvalues and reorthogonalizes the reduced basis. If you want to retain modes with negative eigenvalues, define the environment variable MDI_MNFWRITE_OPTIONS.

  • On Linux platforms type the following command: 

    setenv MDI_MNFWRITE_OPTIONS negative_roots_OK

  • On Windows platforms type the following command: 

    set MDI_MNFWRITE_OPTIONS=negative_roots_OK

In this case the translator will treat modes with negative eigenvalues in the same manner as all other modes.

Command Summary

abaqus adams  job job-name substructure_sim filename length length-units-name mass mass-units-name time time-units-name force force-units-name adams_mnf_block_16 { I Q }

Command Line Options

job

This option specifies the input and output file names to use during results translation. The job-name value is used to construct the default substructure SIM database file name, job-name.sim. The output modal neutral file is given the name job-name.mnf.

If this option is omitted from the command line, the user will be prompted for this value.

substructure_sim

This option specifies the name of the substructure SIM database (.sim) file if it is different from job-name.sim. The file will usually be named job-name_Znn.sim.

length

This option specifies the length units for the model. The valid options are as follows:

  • m, meter, meters
  • mm, millimeter, millimeters
  • cm, centimeter, centimeters
  • km, kilometer, kilometers
  • in, inch, inches
  • ft, foot, feet
  • mile, miles

This option can be defined in the Abaqus environment file as follows: 

adams_length_units=length-unit
mass

This option specifies the mass units for the model. The valid options are as follows:

  • kg, kilogram, kilograms
  • mgg, megagram, megagrams, tonne, tonnes
  • gram, grams
  • lbm, pound, pounds, pound_mass
  • uston, ustons, us_ton
  • klbm, kpound_mass
  • ozm, ounce, ounces, ounce_mass
  • slug
  • slinch, dozen_slug

This option can be defined in the Abaqus environment file as follows: 

adams_mass_units=mass-unit
time

This option specifies the time units for the model. The valid options are as follows:

  • s, sec, second, seconds
  • ms, millisecond, milliseconds
  • min, minute, minutes
  • h, hr, hour, hours

This option can be defined in the Abaqus environment file as follows: 

adams_time_units=time-unit
force

This option specifies the force units for the model. The valid options are as follows:

  • n, newton, newtons
  • kn, knewton, knewtons, kilonewton, kilonewtons
  • mn, millinewton, millinewtons,
  • un, micronewton, micronewtons,
  • nn, nanonewton, nanonewtons,
  • kgf, kg_force, kilogram_force
  • lbf, pound, pounds, pound_force
  • ozf, ounce, ounces, ounce_force
  • dyne, dynes
  • klbf, kip, kips, kilopound, kilopounds, kpound_force

This option can be defined in the Abaqus environment file as follows: 

adams_force_units=force-unit
adams_mnf_block_16

This option defines the contents of the mode shape transformation in block 16 of the modal neutral file. It is meaningful if stress/strain calculations are done following a dynamic analysis in the Adams solver. If the basis for these calculations is modal stress/strain on the modal neutral file, set adams_mnf_block_16=I. This behavior is the default. If the calculations use stress/strain stored in the ODB, set adams_mnf_block_16=Q.